I have a laminate model where the part is of a complex shape. I want to check the shear stresses stresses each lamina as the inter-laminar shear strength is quite low.
In the Postprocessing Data toolbox I have selected Shear XY stresses in the Contour Field. My question is whether the contor plot that I see is in the element co-ordinate system or the the Global Basic Rectangular co-ordinate system?
I tried transforming the co-ordinate system to the matlerial co-ordinate system, however I did no see any difference that is noticeable.
Can someone please clarify this for me.
You may need to do a test model, because the docs aren't immediately clear.
But firstly, you mention Shear ZX... is this a solid composite or a plate element composite? If you are using plate elements, the results can never be in Global Basic coords. Plate results output are either with respect to the local X direction of the element (which has no relationship to the Global Coords), OR they are with respect to the element material coord direction (MCID). I looked at the Nastran docs and could not find a quick answer, so a 5 minute test model is the easiest way for you to check.
If you tranformed to the material coord (MCID) and the results did not change, then either your local plate X directions happen to align with the MCID, OR Nastran outputs results with respect to the MCID. That is the simple test which needs to be run (ie. rotate the MCID in a simple cantilever plate test and see what happenswhen you re-run the results).
The application I am looking at is a composite layup that follows a curved surface. In composite applications, the things to check would be:
1) If the stresses in each ply are below the allowable
2) Interlaminar stresses
However, in composites direction 1 has different material allowable than direction 2. Therefore, I need to know exatly what I am looking at (especially when the part has a complex geometry).
For interlamilar stresses, I used failure indices to determine potential failure locations.
So, I had to transform the results in the material direction. The default direction is Diagonal Bisector for 2D elements (This can be changed from File-> Preferences -> Geometry/Model tab -> Element Orientation).
Once I transferred the results in the material co-ordinate sysytem, I compared my X and Y normal stresses against the direction 1 and 2 tensile/compression allowables. I compared the shear XY against the shear allowable.
You are absolutely correct that for 2Dmodels you cannot have all 3 shear stresses - namely XY/YX/ZX.
Also the reason the result wasn't showing any noticeable differences was because I had the output as a contor plot. A criterian plot is much better to use in such situations.
I hope this helps other users with similar problems.
I have a follow up question in addition to what EndZ has mentioned.
Suppose lets say you have a laminate as follows:
The above pic ( I picked it up from an Applied CAX presentation file) shows how FEMAP will assign ply orientation wrt material angle for the entire laminate.
What is unclear to me is that if you choose material angle/direction in the contour output transformation and select each ply, will Femap transform the result to local principle axes of each ply or will it transform the output wrt to overall Laminate Material Angle?
I hope my question is clear.
I will have to do a simple test for a 3 ply laminate and verify the above via hand calc. May do it this weekend.
From several experiments, I have deduced that Element X axis does not always coincide with the Material Co-ordinate system. If they were the same, the results should be identical when viewing the contour plots. However transforming the results from the default co-ordinate system (Diagonal Bisector) to the Material co-ordinate system, there is change in the contour plot.
So far, this is what I have concluded:
When working with composites, the co-ordinate system must be changed to the material co-ordinate system to accurately compare the stresses against the allowables.
In simple shapes (eg:- flat panels) the material co-ordinate system might align with the default co-ordinate system. However, one should still verify that or better transform the results in the material co-ordinate frame.
I believe that when the results are transformed to the MCID, the results are relative to the material angle for the entire laminate. So when to set the Material Orientation (Modify -> Update Element -> Element Orientation) you are setting the material angle for the laminate.
Now if you place a 0 degree UD tape the fibres will aling to this axis. A 90 degree UD will have the fibres orientated 90 degrees to the orientation you specified. So you can use Normal X and Normal Y stress plots to see how much the fibres are getting stressed.
The tricky part is for 45 degree plies there is no way to compare the stresses in the X or Y direction of the fibres.
I am fairly new to composites so I am not sure what the best practices are. A video tutorial from an expert covering this would be greatly appreciated.
It seems that transforming stress output vectors to MCID, will orient itself to ply local axes. Although I am getting way off results for Y normal stresses of plies.
Will post detailed summary tomorrow along with contour pictures.
In the mean time, perhaps a more experienced person with composites could chip in?
Sorry, I don't think I was being clear enough to be helpful.
Whenever using composites, the material coordinate (MCID) must be set. I can safely say the MCID is unlikely to be the same as the element X axis, except just by coincidence in the very simplest cases.
Independently of Femap, NX Nastran produces results for CQUAD elements. For anything without an MCID, "X" results are most definitely output in the element X axis (defined by diagonal bisector). When an MCID is set, the NX NASTRAN X direction results might be defined by element X axis (diagonal bisector), OR by MCID X direction projected on to the element. This is what needs to be determined with absolute confidence (and I was hoping a composites specialist would simply step in and confidently declare one of: "MCID projected X", or "Element X")
Unfortunately, just doing the transform in Femap with a change in contour is not enough on its own to make the judgement, unless you are very clear on what exact result you are expecting to see. The transform (and also no transform) relies on the base assumption of what the reference X direction actually is for the output NX Nastran results. Femap defaults to element bisector for quad elements... the question is whether that default remains correct for CQUAD elements with a material direction MCID defined.
Anyway, I have done a simple test... the answer is that despite setting an MCID, NX Nastran's default behaviour is to continue to define an X direction result on a CQUAD element based on the diagonal bisector, not the MCID. Thus, Femap's default assumption (diagonal bisector) remains OK as the reference X direction for results where an MCID has been set for CQUAD elements.
This also concurs with Remark 7 of the CQUAD4 entry in the NX Nastran Quick Reference Guide...
BUT if you happened to be using QUAD8 elements, then the local X direction for results is no longer the diagonal bisector (relevant for elements which are non-square or non-rectangular)!
Just to be clear, I think my & EndZ queries are completey different.
I am more concerned with how Femap will interpret output vector transformation in to MCID for composite laminate plies whose orientation is different from 0 deg.
I think EndZ is more interested in finding out how NX Nastran will interpret elemental CID when Femap assigns a MCID.
I will post my findings of my concern once I get some time tomorrow.